Allegro PCB Tutorial

This tutorial should be helpful for doing simple PCB designs using Allegro PCB editor. One very good reference for the basics of the tool is Complete PCB Design Using OrCAD Capture and PCB Editor by Kraig Mitzner.

Step 1 - Schematic
1. Open Allegro Design Entry CIS.
2. Create New Project and add relevant Libraries.
3. (a) Place all required symbols on the schematic page. You may need to create symbols for your custom IC package (Details can be found in the reference book)
(b) Right Click on each symbol and choose "Edit Properties". The "PCB Footprint" property should have a name with the corresponding name.dra file being present in $SPB_HOME/share/pcb/pcb_lib/symbols directory. You may need to create/download footprints and padstacks for your custom IC package (Details can be found in the reference book)
4. Make all connections. Use net labels for readability and unclutered schematic.
5. Save schematic page and project.
6. Select project_name.dsn file in project window and goto Tools>Create Netlist.

(b) For 4-layer PCB. This option is useful if you want impedance control (50 Ohm usually) tracks.

7. Setup>Constraints>Constraint Manager
(a) Electrical--Net--Routing--Impedance--Set the impedances to 50 Ohm for the nets you want.
(b) Physical--Physical Constraints--All Layers--Line Width--Min=8.0 Max=12.0 and Vias=VIA_16MIL:VIA_36MIL
(c) Physical--Net--By Layers--Can individually set line width and vias for individual net. Or default loaded as per (b) above. Good to keep power nets as higher widths and bigger vias.
There are lots of other constraints that can be specified.
8. Add>Line goto Options on the right pane--Line lock-90, Line width-10.0, Class-Board Geometry, Subclass-Outline.
Draw the line to form a closed rectangular area. This will be the physical outline for the PCB.
9. Add>Rectangle--Options--Class-Route Keepin, Subclass-All. Draw the rectangle 4 grid point inside the outline.
10. Add>Line--Options--Line lock-45, Line width-10.0, Class-Board Geometry, Subclass-Silkscreen Top. Draw the line to form a closed rectangle with 45deg lines at corners 5 grid point inside the outline. This should serve as your logical boundary of the PCB. All items and routing need to be done within this.
11. Place>Quickplace (If you do not have too many components in the design). Recommended is to do Place>Manually. Then you can select each component individually and decide on its placement.
12. Route all the nets. You will automatically get DRC errors as red flags while routing. You should use only Top and Bottom Etch layers for routing.
13. For 4 layer board the in between planes are for VDD and GND which need dynamic copper fills. Shape>Rectangular--Options--Class-Etch, Subclass-Power/Ground, Type-Dynamic copper, Assign net name-vdd!/gnd! Then draw the rectangle covering your full design but inside the area drawn in 10 above.
14. If you want to add any text on the PCB for reference. Add>Text--Options--Class-Board Geometry, Subclass-Silkscreen Top/Bottom depending on where you want the text to appear, Text Block-according to size needed. Then point at the place and start typing. You may need to Mirror the text if writting to bottom layer.
Now we are done with the design and need to check the PCB for completeness and generate the Artwork for manufacture. Step 3 - Manufacture
1. Check the following reports to ascertain there are no errors in the design
(a) Tools>Quick Reports--Dangling Lines Report
(b) Tools>Quick Reports--Design Rules Check Report
(c) Tools>Quick Reports--Unconnected Pins Report
(d) Tools>Quick Reports--Unplaced Components Report
Rectify if any errors pop up in these reports.
2. Add>Rectangle--Options Class-Manufacturing, Subclass-Photoplot_Outline Draw the rectangle outside the board outline drawn in Layout/8 above.
3. Manufacture>NC>NC drill used to generate drill file if needed.
4. Manufacture>Artwork
(a) General Parameters--Device Type-GerberRS274X, Format--Integer-5, Decimal-5
(b) Film Control--Populate all the required films

(c) Create Artwork
5. Compress all the .art files and the .drl file into a zip file and send to your PCB manufacturer.